CFD case studies on Stop Valve, Pressure Reducing Valve, Safety Relief Valve, Valve Cavitation
By
Dr. Sharad N. Pachpute
Scope of CFD Modeling for Valve Design
 Flow Control valves are important components of process industry systems, power plants, water or gas pipelines cities, and many hydraulic devices. They play a crucial role in controlling the fluid flow
 There are a variety of valve designs that are designed depending on industrial applications. Valves are commonly used for safety purposes in flow control systems. When they are used for flow control, the flow dynamics of the valve need to match the flow dynamics of the entire flow system
 The relation between valve position and the pipe system shows that the pressure drop and flow rate are highly nonlinear.
 CFD users need to understand the following subjects
 Basic of CFD modeling and numerical schemes
 Turbulent Modeling: Flow across the valve is turbulent. We have to select appropriate turbulence models
 Multiphase flow modeling: Due to cavitation or gas bubbles in liquids, multiphase models like the volume of fluid methods need to select in numerical simulations
.
 Pressure variations for various types of valves for a fixed pressure drop are shown below. It is observed that the local pressure within the valve is same for all the four valves. The low pressure can cause cavitation if liquid flows through the valve
 The operating conditions may cause damage or high maintenance costs. The damaged valves can create safety hazards for the plant personnel.
Cavitation and Choking
 The valves at high temperature and highpressure drop applications are prone to cavitation and choked flow
 The location and type of valve are important for liquid flow in industrial or commercial applications
 The following figure shows Severe pitting damage due to cavitation on the valve body of a Vnotch ball valve which is used to regulate the cooling water flow
 The volumetric flow rate at choked conditions is the maximum that can be obtained for the given inlet conditions and cannot be increased irrespective of how much the pressure drop across (∆P) the valve is decreased or increased
CFD Modeling for Valve Design
 CFD Modeling can help to design and find the optimum pressure drop to avoid the problem of cavitation and choking as well as vibration caused by high velocity
 Computational fluid dynamics (CFD) has shown good promising results in the last decade for complex flows. CFD modelling of valves predicts well internal flow pattern and pressure drop. The effect of valve movement, change in operating conditions, cavitation and choking are studied numerically with the help of CFD models
 Based on CFD results of fluid flows and FEM analysis of solid, engineers optimize the design parameters for hydraulic components
 A suitable valve for given operating condition in flow systems can be designed as per industrial applications
CFD Modeling of Globe Valve
Globe (stop) Valve
 Globe valves are commonly used in process industries
 CFD analysis of stop valve carried out by Yang et. al (2011) is presented in this section
Computational Domain
 The CFD domain is selected such a way that the valve body is at a distance of 10D from the inlet and outlet boundaries
 the inlet and outlet of the valve), velocity and pressure conditions were specified
Mesh Model
 The mesh was created using Gambit with 1.2 million cells
Details of Boundary conditions and CFD Modeling
 The flow inside the valve and pipeline is considered to be unsteady that is the major factor to cause vibration and flow induced the noise
 Inlet was specified with velocity outlet as pressure outlet
 The RNG kε model was selected to simulate turbulent flows
 To analyze the pressure oscillation, the sound pressure level is calculated as
Where, p represents the pressure, p_{0} is the reference sound pressure
 The sound pressure level calculated with respect to time for different location of the pipe and valve is obtained as frequency spectrum of the pressure fluctuation by FFT analysis. This method is used to calculate the vibration caused by fluctuations inside the pipe and valve body
CFD Results
 The variations of pressure and velocity, flow pattern are shown below
 The trend of the pressure fluctuation for different velocities is analyzed, the result shows that the fluctuation in magnitude of pressure wake increases as velocity increases
CFD Modeling of Pressure Reducing Valve
 Pressure reducing valve is widely used in thermodynamic system to control the pressure of superheated steam
 MultiStage High Pressure Reducing Valve (MSHPRV) is one of commonly used pressure reducing valve
 This valve has low noise, vibration and less energy consumption
 CFD analysis of Safety Relief Valve carried out by Chen et al. (2018) is presented in this section
CFD Model of MSPHRV
 Meshing MSHPRV: ANSYS ICEM CFD was used to create the structured and unstructured mesh
Details of CFD Modeling
 Mach number is the parameter to account the compressibility in fluid flow
 The fluid with a higher Mach number can result in aerodynamic noise and energy consumption
 The relationship between Mach number and the flow parameters pressure, local velocity, Mach number and crosssectional area
 Transmission loss at inlet and outlet is important for acoustic performance
 In the acoustic calculation, the sound pressure (p) is a complex number
 In order to facilitate the calculation,
 Transmission loss (db) at inlet and outlet
 FEM method was adopted to carry out acoustics analysis
 RNG kε turbulence model was used for simulation as this model considers the effects of rotation and curvature of wall
 The turbulence was combined with a compressible gas model for the fluid flow through MSHPRV
 Turbulent dissipation rate (ε) is considered to characterize the energy consumption resulted from turbulent flow
 For MSHRPV, the larger of exergy loss is accounted with larger of energy consumption
Boundary Conditions
ANSYS FLUENT was used for numerical simulation and the following boundaries were set
 Inlet was specified with pressure inlet at 16 MPa and temperature of 813.15K
 Wall considered as noslip boundary
 Symmetry for midplane of CFD model
 Outlet specified with pressure outlet
CFD Results
 From the numerical simulation, Mach number, turbulent dissipation rate and exergy loss in MSHPRV obtained
 The fluctuations in the valves are reduced for fourstage pressure reduction valve
 Mach number distribution with different structural diameters of perforated plate is given below
CFD Modeling of Safety Relief Valve (SRV)
 Safety relief valves are commonly in power plant industries used to open and relieve the excess pressure , to stop and open the flow till the normal situation is obtained
 There are two types of safety relive valve: 1) pilot operated, 2) direct operated (spring loaded)
 Numerical study of Safety Relief Valve carried out by Song et al. (2014) is presented here
CFD modeling and motion of valve disc
 The motion of the valve disc is computed using Newton’s second law of motion
Where m is the combined mass of disc, disc holder and stem

 In above equation, the first term on the right side represent the viscous and pressure force acting on the disc in Ydirection due to flow
 The second term is the spring force in the Ydirectin
 The last term (G_{disc}) is combined weight of disc assembly, but it is neglected as it is small compared to other forces
 Moving mesh technique was used to consider the motion of disc
 Mesh Model was created in ICEM CFD
 Boundary conditions are set in the following way
CFD Results
 CFD results show that the air accelerate through the SRV valve. Hence, the Mach number is maximum
 Contours of Mach number and absolute velocity
 Velocity vector in the midplane of the valve section
Modeling of Valve Cavitation
 Cavitation often appears in many kinds of control valves during the actual operation process
 Dimensionless numbers of cavitation number (σ) and cavitation index (σ_{v}) are used to assess the proneness to cavitation
Where P and v are pressure and velocity at the reference location. P_{v} is the saturated vapour pressure. P_{u} and P_{d} are the pressures at upstream and downstream of valve.
CFD Modeling
 CFD modeling carried out of flappernozzle valve by Li et. al ( 2013) is presented
 To model the cavitation phenomena at inlet velocity, the set of following equations are solved in numerical simulations
 Based on the ensemble averaging of the Navier–Stokes equations, flow equations for a twophase mixture are obtained for CFD Modeling of cavitation
 The governing equations for mixture models are given in the following forms
Continuity equation:
Momentum transfer equation:
Turbulent kinetic energy equation:
Turbulent dissipation equation:
Turbulent Viscosity:
Vapor mass transport equation:
In the above equation, f_{v }is the vapor mass fraction, Re_{v} is the vapor generation and R_{c} is the condensation rate. If f_{g} is the noncondensable gas fraction, then Re_{v }and R_{c} are calculated as
 The effect of turbulence is considered in the full cavitation model by raising the phase change threshold pressure value
where P_{t }= 0.39K
Computational Domain
 CFD Model of the flapper–nozzle assembly is given as below
 Boundary conditions: inlet velocity (21.2 m/s), outlet pressure and noslip condition walls.
Mesh Model
 Mesh created in Gambit with around 0.51 million TGrid elements
Numerical Details
 Body force due to gravity is considered
 Pressure–velocity coupling: SIMLPEC scheme
 Pressure discretization: PRESTO! scheme
 Momentum, k and ε : First order upwind
 Volume fraction QUICK
CFD Results
 Cavitation phenomenon based on experimental and numerical results is compared for nozzle inlet velocity 21.2 m/s
 CFD results show the formation of cavitation at the exit of nozzle.
 CFD results compare well with experimental results
References
 Q. Yang, Z. Zhang, M. Liu, J. HU, Numerical Simulation of Fluid Flow inside the Valve, Proceeding Engineering, 23(2011)53550
 X. Song, L. Cui, M. Cao, W. Cao, Y.Park, W. M. Dempster, A CFD analysis of the dynamics of a directoperated safety relief valve mounted on a pressure vessel, (2014)
 X. Song, L. Cui, M. Cao, W. Cao, Y.Park, W. M. Dempster, A CFD analysis of the dynamics of a directoperated safety relief valve mounted on a pressure vessel, Journal of Agriculture, Science, 231239 (2011)
 A. D. Toro, Computational Fluid Dynamics Analysis of Butterfly Valve Performance Factors, Master thesis, Utah State University (2012)
 F. Q. Chena, J. Qian, M. Chena, M. Zhangc, L. Chenc, Z. Jina, Turbulent compressible flow analysis on multistage high pressure reducing Valve, Flow Measurement and Instrumentation 61 (2018) 26–37
 J. Qian, Z. Gao, C. Hou, Z.Jin, A comprehensive review of cavitation in valves: mechanical heart valves and control valves, BioDesign and Manufacturing (2019) 2:119–136
 S. Li, N.Z. Aung, S. Zhang, J. Co, X. Xue, Experimental and numerical investigation of cavitation phenomenon in flapper–nozzle pilot stage of an electrohydraulic servovalve, Computers & Fluids 88 (2013) 590–598
You explain each and everything in very clear manner. Beautiful Blog.
Thanks for your comment.
These are truly great ideas in concerning blogging.
You have touched some fastidious factors here.
Any way keep up wrinting.
Could please provide any detail about how the code should look like (CEL) for the moving mesh in the Pressure Relief Valve?
Very didactic. Nice graph and images. Very friendly